Author Topic: easy PCB dipoles for 433, 868 and 915MHz  (Read 29687 times)

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #45 on: March 05, 2017, 07:15:33 AM »
My results with your dipole and a long (l/2) coax to the board have been great. But as soon as I mount the antenna close to the espgw board I get significant noise. I've been working on a new version of my gateway to address these issues. Two of the changes I've made might be interesting to you:

1.) I decided to use a balun with the dipole to try and get better noise immunity. I settled on the HHM1522A7 (https://product.tdk.com/info/en/documents/data_sheet/rf_balun_hhm1522a7_en.pdf) for 868 mhz.  The reason I think it might help is that without it the outer surface of the coax and the ground plane of the board acts as third leg of the antenna, distorting the radiation pattern and providing an easier path for ground noise pickup.

2.) I'm going to mount the dipole perpendicular to the PCB to keep the orientation of the fields the dipole can pick up perpendicular to any noise the esp might generate. To do so I have a cutout at the end of the PCB into which I'll insert the dipole. Then I'll solder onto the SMA pads on both sides. So I appreciate their presence in your design.

Joe

captcha

  • Full Member
  • ***
  • Posts: 108
  • Country: au
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #46 on: March 06, 2017, 04:57:06 AM »
Thanks for the feedback, what I've got so far is:

> issue an updated version of the existing dipoles design that
    - has a bend radius instead of a 90 degree angle
    - reduces excess area on the SMA solder pads
    - has a 50 Ohm impedance for the short microstrip feedline between the SMA connector and the dipole
    - is re-checked for resonance on 433/868/915MHz

> issue two new designs:
    #1: direct solder-on pads (through-holes)

    #2: with pads for u.fl connector


For all designs:
  - minimise overall dimensions
  - issue as:
         - three-combo (433 with cut marks for 868 and 915MHz)
         - two-combo (868 with cut marks for 915MHz)
         - dedicated 915MHz


Then some points of interest.

The vias as shown in ChemE's post with the picture of the surface mount board is intriguing but should also raise a concern with feedline purists. Vias and through-holes in feedlines may be helpful for rigidity, but may also cause unwanted detuning and reflections because they are 90 degrees to the signal path. From what I've read I'm not so much concerned with reflections but I know that something like a tuned stub can be used a as an impedance match. The thickness of the pcb even at 915MHz probably still isn't large enough to be a significant portion of a wavelength but it is 'sticking out' somewhat. For sub GHz designs I think we can put this one to rest and just use vias and through-holes in most locations.

I've noticed that the SMA footprint is somewhat on the large side. I would like to shorten it and thin it out a bit, but keeping in mind to aim for 50 Ohms track impedance. Joe, you mentioned that you use the SMA pads to solder your board at a 90 degree angle to it. Will it jeopardize this feature for you? Can you comment on the freedom I have to change the geometry of the SMA pads? I think it's probably best for me to work out the dimensions for 50 Ohms first and then present here so you can see what it's going to look like first.

For the SMA connector design, I'd like to round the beginning of the dipole element tracks from the feedline somewhat. Not so much for concerns of reflections but more for trace flexibility because of the relatively small and flexible pcb. I'll try the 'Trace Curvature Radius >= 3 Trace Width' approach and see how that goes. This is obviously of no concern for the solder-on design but maybe for the u.fl connector. With regards to the latter, Mark, can you advise whether you want the u.fl right in the middle or slightly on the side with a bit of microstrip like the current design? I guess if it's in the middle the width could come down dramatically but you may want some holes next to the coax to secure it in place.

Meandering dipoles.. verrry interesting, but way down the list for me, haha.. Thanks for the link though.

Any other suggestions?

captcha

  • Full Member
  • ***
  • Posts: 108
  • Country: au
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #47 on: March 06, 2017, 05:41:38 AM »
Quote from: joelucid
..as soon as I mount the antenna close to the espgw board I get significant noise.

Ooh, that's not good. Only on receive or on tx as well?

Quote from: joelucid
1.) I decided to use a balun with the dipole to try and get better noise immunity. I settled on the HHM1522A7 (https://product.tdk.com/info/en/documents/data_sheet/rf_balun_hhm1522a7_en.pdf) for 868 mhz.  The reason I think it might help is that without it the outer surface of the coax and the ground plane of the board acts as third leg of the antenna, distorting the radiation pattern and providing an easier path for ground noise pickup.

You got it. The GND tracks of your espgw board WILL form part of the antenna, the trick is to a) minimise the amount of noise the antenna picks up from your board when it's receiving and b) minimise the effect of a radiating antenna on your board.

Also consider 'unintentional' antennas such as powersupply leads and other wires. At these frequencies almost anything acts as an antenna. It would be interesting to see if you can get even better immunity by adding small toroids to wires and by metal-shielding your espgw board.

The balun you found adds some losses but definitely helps to isolate common mode current caused by the (hopefully small) asymmetry of the dipole. I think you're on the right path, I just chose not to include this component in my design. However, I'd love to see some numbers when you've finished testing with the balun. It could be a great addition for those who want to experiment with antenna designs and I think it's a worthwhile path of investigation.


Quote from: joelucid
2.) I'm going to mount the dipole perpendicular to the PCB to keep the orientation of the fields the dipole can pick up perpendicular to any noise the esp might generate. To do so I have a cutout at the end of the PCB into which I'll insert the dipole. Then I'll solder onto the SMA pads on both sides. So I appreciate their presence in your design.

Are you saying that initially the coax feedline was not straightened out but maybe somewhat curled up? Then what you're seeing is expected behavior. Dipoles are very prone to picking up noise within a short distance of it. Not sure if this is purely within the near-field or just within the first half-wavelength.

Another point of interest is that, even with an isolation transformer, if your coax is not straight and perpendicular to the dipole for at least a half wavelength, it will very easily pick up rf on the outside of the coax when the antenna is transmitting.

However, if you're going to mount your espgw right at the feedoint of the dipole you may be asking for trouble. Without any shielding, you're putting your board right in the 'hottest' field of the antenna. I'm not saying it can't be done but if you're already having noise problems *with* a feedline, putting the gw board right on top of the dipole may make it worse. For your sake I hope you can prove me wrong! haha.. :-)

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #48 on: March 06, 2017, 11:00:01 AM »
Quote
Ooh, that's not good. Only on receive or on tx as well?

I haven't looked at tx. It's the receiver sensitivity that I'm currently optimizing.

Quote
Are you saying that initially the coax feedline was not straightened out but maybe somewhat curled up? Then what you're seeing is expected behavior. Dipoles are very prone to picking up noise within a short distance of it. Not sure if this is purely within the near-field or just within the first half-wavelength.

I'm working on an enclosure for the GW (now that Tom's initiated me to 3D printing ;)). For ease of manufacturing at first I tried a dipole where the lower half is the circuit board (gnd plane as lower leg). That is very noisy.

A dipole connected with a very short feed line has the same problem to a lesser extent -and without balun that's kind of clear: even with the pcb perpendicular you now have an unintended L dipole which efficiently picks up noise.

Quote
Another point of interest is that, even with an isolation transformer, if your coax is not straight and perpendicular to the dipole for at least a half wavelength, it will very easily pick up rf on the outside of the coax when the antenna is transmitting.

However, if you're going to mount your espgw right at the feedoint of the dipole you may be asking for trouble. Without any shielding, you're putting your board right in the 'hottest' field of the antenna. I'm not saying it can't be done but if you're already having noise problems *with* a feedline, putting the gw board right on top of the dipole may make it worse. For your sake I hope you can prove me wrong! haha.. :-)

I've got the pcb partitioned so that the esp8266 is as far away from the antenna as possible and I've added just about every trick I could find in app notes on EMC - short of shielding (beyond via shielding) and doing a 4 layer board. We'll see how it turns out.

The power line is a problem since the enclosure is a cylinder with the pcb horizontally in the middle, vertical dipole. So the power cable needs to go down to the bottom parallel to the dipole. I've been told I can avoid any impact on the antenna by shielding the cable with ferrites.

Joe

perky

  • Hero Member
  • *****
  • Posts: 873
  • Country: gb
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #49 on: March 06, 2017, 01:33:31 PM »
The single most important thing for reducing radiated EMI is ensuring that at the point of PCB exit there is a low an RF impedance as possible between the digital ground and chassis ground, and that every I/O signal that exits a PCB has an EMI filter (usually using a ferrite and a small capacitor, and often an ESD protection diode has enough capacitance so both EMC and ESD are covered). If a metal box is used as chassis ground this means very fat and short connections as close as possible to each I/O connector, even a few mm of thin wire will have significant impedance at GHz frequencies and this will allow noise to exist between chassis and digital grounds. The low RF impedance of ground and chassis eliminates common mode noise, the filters eliminate differential noise. The next thing is to ensure all I/O is, if possible, sited along one side of the PCB only to stop a dipole effect of the signals exiting the board (this includes the antenna). Of course you also need to properly filter power supplies and use pi filtering for any high speed switching parts like an MCU and the radio on board, and use low leakage and low stray capacitance layout techniques for switching regulators. It goes without saying a solid ground plane is a must to reduce impedance.

If battery operated then chassis ground == digital ground, in which case the position of the connectors all down one edge of the PCB will have a signifcant EMI reduction impact.

Mark.

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #50 on: March 06, 2017, 02:11:44 PM »
My enclosure is 3d printed, so there's no metal chassis.

From what I have debugged so far I think the culprit is the esp-12e module. It's built on a 2 layer board and the flash chip isn't separately decoupled. Decoupling caps don't go down down into the pF. The signal return paths for the flash seem pretty long to me since there isn't a ground plane. There's a shield on top, but that doesn't fully enclose the module due to lack of ground plane and the i/o pins aren't filtered.

On top of what I said above my new design filters all IO and power at both the RFM and the ESP, uses a almost completely continuous ground plane with just a couple of very short bridges and ground areas on both sides are heavily stitched with vias. We'll see if it's enough.

If it doesn't one could look at shielding the esp-12e or doing away with the module and integrating the esp8266ex directly on a 4 layer board with the rfm. Any other ideas?

Joe

perky

  • Hero Member
  • *****
  • Posts: 873
  • Country: gb
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #51 on: March 06, 2017, 05:23:19 PM »
That theory fits, it appears to be near field (primarily H-field I would say) coupling with your antenna which is what you'd expect if there are large current loops going on.

Looking at the layout of the esp-12e it does have a guard rail all the way around the can (tacked at every pin location) tied to ground at one point. That's not ideal but not a disaster, it'll still work as a shield especially to E-fields. However as you say the underside is essentially full of holes.

Do you fit other components on the opposite side of the esp-12e? Can you put a solid ground plane underneath it somehow?

Mark. 

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #52 on: March 06, 2017, 05:38:06 PM »
Quote
Do you fit other components on the opposite side of the esp-12e? Can you put a solid ground plane underneath it somehow?

No - the ground plane on the bottom is almost solid. The top side also has lots of copper and its all via stitched together. I'll attach the current design. Disregard the sizing of the pass thru caps, I haven't done those yet.

Joe

perky

  • Hero Member
  • *****
  • Posts: 873
  • Country: gb
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #53 on: March 06, 2017, 06:07:25 PM »
Well I would say you've done just about all you can for shielding of the esp-12e ;). My guess now is that the proximity of the antennae means the rf transmitted from the esp-12e is de-sensitizing the RFM69HCW. Since it's OK with the RFM69HCW antenna some distance away it doesn't appear to be a lack of shielding over that. So can you turn the power of the esp-12e right down so all the rest of the logic being exercised but just not transmitting much rf, and does that help?

Edit: Maybe it's worth putting on a 915MHz bandpass filter inline close to the RFM69HCW? Something like this:
http://www.digikey.co.uk/product-detail/en/johanson-technology-inc/0915LP15B026E/712-1122-1-ND/1560951

Mark.
« Last Edit: March 06, 2017, 06:43:05 PM by perky »

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #54 on: March 07, 2017, 06:37:08 AM »
Quote
So can you turn the power of the esp-12e right down so all the rest of the logic being exercised but just not transmitting much rf, and does that help?

Interestingly noise doesn't correlate with Wifi activity of the esp8266. But it does correlate with activity on the flash SPI bus. If I just measure noise and tickle the ESP's wdt to avoid reboot there's little noise. But as soon as I call yield the ESP starts paging in program code from the flash and the noise is back.

This makes sense as the flash isn't properly decoupled and the flash signal loops aren't very low impedance. Any E fields will likely be shorted away in the new design. But the H fields continue to be a concern. I have some ferrite plates here so when its assembled I'll try shielding the H fields that way to see if it helps.

Joe

perky

  • Hero Member
  • *****
  • Posts: 873
  • Country: gb
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #55 on: March 07, 2017, 08:25:32 AM »
OK. Since you don't use the SPI pins (you've just got AC terminators on them), maybe changing it for a ESP-12S and add the central ground pad is a possible way forward (this apparently has an "improved PCB layout" and "better radio performance"). Maybe this lack of ground plane was a real issue with the 12E.

BTW have you tried it without the termination components fitted? I'm just wondering whether this forces SPI currents outside of the module shield area.

Mark.

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #56 on: March 07, 2017, 08:55:45 AM »
Quote
maybe changing it for a ESP-12S and add the central ground pad is a possible way forward (this apparently has an "improved PCB layout" and "better radio performance"). Maybe this lack of ground plane was a real issue with the 12E.

Excellent suggestion!  I hadn't see this module. I'll get some to try out.

Quote
BTW have you tried it without the termination components fitted? I'm just wondering whether this forces SPI currents outside of the module shield area.

Yeah, that's the way it is now. The design I posted I haven't received yet so I don't know how it will perform. I did add termination components to the old gw on the SPI lines during debugging. First just 47pF to gnd without a resistor which made things worse (understandably since this is a RF short). With 200 Ohm added things were unchanged from without termination.

Joe

ChemE

  • Sr. Member
  • ****
  • Posts: 402
  • Country: us
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #57 on: March 08, 2017, 09:00:26 AM »
...Velocity factor for a lot of coax is around 0.66 so that should be all you need to determine how long the feedline needs to be.

As an example for 433MHz:
- Full wave in free space: 300 / 433 = 0.692 m (69.2 cm)
- Half wave: 69.2 / 2 = 34.6 cm
- Compensated for 0.66 velocity factor of RG-174 coax: 34.6 x 0.66 = 22.9 cm

So doing the math for 915Mhz, we end up at 108mm for our feedline length.  It looks like these UF.L to SMA patch cables are cheap and readily available on Ebay but only in lengths that are multiples of 5cm.  10cm patch cables are $1.50 shipped from China for instance.  Is the patch cable being short or long by as much as 2.5cm anything to get excited about?  In the case of 915MHz the mismatch is only 0.8cm which I'm betting is insignificant but I would like to understand the theoretical implications since I'm attempting to make the lowest noise gateway that I can.

EDIT:
Looking at the pictures from the auction perhaps the error is even smaller than I thought.  The connector adds 10mm making this 2mm too long assuming that the connector counts.


EDIT 2: I suppose I could set my center frequency to 900MHz (11cm ideal feedline) and see if there is any statistically significant difference in RSSI when compared to a center frequency of 915MHz (10.8cm ideal feedline).
« Last Edit: March 08, 2017, 09:15:14 AM by ChemE »

captcha

  • Full Member
  • ***
  • Posts: 108
  • Country: au
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #58 on: March 10, 2017, 12:16:04 AM »
The connector counts.

Ideally you want the whole assembly mounted/screwed in/attached/stretched out and then measure the distance between antenna feed point and the radio's antenna port.

I've ordered some u.fl surface mount connectors and will position it right in between the dipole elements. That should minimise any additional paths from the connector to the antenna elements.

joelucid

  • Hero Member
  • *****
  • Posts: 869
Re: easy PCB dipoles for 433, 868 and 915MHz
« Reply #59 on: March 18, 2017, 06:03:20 AM »
Quote
Excellent suggestion!  I hadn't see this module. I'll get some to try out.

Got the components (including the ESP-12S) and the new boards and soldered everything together. These feed through caps certainly are a pain to solder. But the results speak for themselves:

Noise level (at 55khz settings) measured just tickling the WDT:

Noise level, Percent of detections
-107.5,  10%
-108.0,  20%
-108.5,  70%
-109.0, 100%

Noise level measured with flash SPI active:

Noise level, Percent of detections
-107.5,  10%
-108.0,  30%
-108.5,  90%
-109.0, 100%

So they are now really the same and both are great and similar to a dipole connected via long coax. Now the real work begins: identifying which of the many changes actually fixed the issue. And of course build the enclosure.

Joe